SOLIDWORKS Toolbox Settings Overview
SOLIDWORKS Toolbox administrators can use the Toolbox Settings tool to select and customize hardware as well as set user preferences and permissions. The best practice is to configure SOLIDWORKS Toolbox before using it.
To launch the SOLIDWORKS Toolbox Settings tool:
- In Windows, click Start > SOLIDWORKS Tools version > Toolbox Settings
- In SOLIDWORKS, click Configure in the SOLIDWORKS System Options > Hole Wizard/Toolbox dialog box.
- If Toolbox is managed by SOLIDWORKS PDM, click Yes at the prompt to check out the Toolbox folder. If you click No or if you do not have permission to check out the Toolbox folder, you can view Toolbox settings but you cannot save changes. To learn more about managing SOLIDWORKS Toolbox in PDM, review our guide How to Setup Toolbox in PDM.
The tool launches to the Home tab with a Welcome to Toolbox Setup dialog.
If the tool was previously locked with a password, users must login in the upper left or changes will not be saved. We highly recommend keeping the password in a safe place as there is no method to recover the password.
The top menu bar also contains quick access to the save and home icons as well as the options divided into 5 categories.
Jump to category:
1) Hole Wizard
Use the Hole Wizard page to configure Hole Wizard standards, types, and holes. You can also assign smart fasteners for each standard hole type. Navigate through standards using the left pane or by clicking folders in the right pane. You can select or clear item checkboxes in the right pane to choose if standard should be displayed to SOLIDWORKS users or not. Deselecting does not delete the standard from the database—the standard is simply turned off.
The left pane is organized by standard, type, and holes. Expand each category to display the options.
To simplify the design process, select standards, types and hole standards only for the hardware that you use. This will reduce the selections displayed to SOLIDWORKS users when using the Hole Wizard. The image below shows the difference between all standard selected and only ANSI Inch, ANSI Metric, and ISO. This streamlines the design process by reducing the number of choices for the designer.
Selecting a specific hole will display the various options to configure that hole as shown below.
- The Smart Fastener assigned to automatically populate for this hole when Smart Fasteners are used in SOLIDWORKS.
- The properties of the hole. These properties will vary depending on the hole selected. The example above contains Sizes, Thread Data, and Screw Clearance tables.
- Clicking a property displays the associated data table. This is where hole size values can be adjusted, existing sizes enabled/disabled, new sizes added (blue plus + icon), or sizes deleted (red X icon).
- Standards can also be exported to an Excel spreadsheet to be modified and then imported back into the Toolbox Settings. When exporting the data, DO NOT modify the exported file’s format in any way or the data will not be imported correctly. DO NOT add or remove columns.
2) Customize Hardware
Use the Customize Hardware page to select standards, categories, types, and components. At the component level you can select component sizes, type property values, and type part numbers. Navigate through standards using the left pane or by clicking folders in the right pane.
You can right-click items in the left pane and perform the following on files in standards folders, categories of standard folders, folders of types of components within a category, or individual component files:
- Cut and paste files, retaining file names
- Copy and paste files
- Delete files
- Insert new subfolders
- Add new files
- Double-click file or folder names to rename them.
These are the standards and hardware components available in the Toolbox located in the SOLIDWORKS Task Pane. Deselecting standards unused by your company will simplify the design process and clean up the user interface.
Selecting a specific hardware component will display the various options to configure. Socket Head Cap Screw is shown as an example below.
- The component’s name and possible configuration quantity. Depending on your Toolbox settings, SOLIDWORKS will either create an additional configuration or an individual part for each hardware combination. Reducing the number of available options will reduce the configuration quantity drastically (see the next image for an example), improve SOLIDWORKS performance and help SOLIDWORKS users be more consistent with the hardware they select.
- The properties available to configure. Each category and component type may have different properties available. For the example image above, you can configure the size, length, drive type, thread length, thread display, thread data, and even the color of the component.
- Custom Properties assigned to this component.
- Detailed values for the component. Company specific part numbers and descriptions can also be added.
- The tables can also be exported to an Excel spreadsheet to be modified and then imported back into the Toolbox Settings. When exporting the data, DO NOT modify the exported file’s format in any way or the data will not be imported correctly. DO NOT add or remove columns.
An example of reducing possible configurations is shown below. With all Drive Types selected (by default), there are 32,988 possible configurations in a single part file. By deselecting all drive types except Hex, the possible configurations were reduced to 9,879.
The image below further reduces the possible configurations from 9,879 to 6,586 by changing the Thread Display options to remove Schematic. Deselecting unused sizes and lengths to allow display sizes available to your company will further reduce the possible configurations and improve SOLIDWORKS performance when working with Toolbox components as well as create a more consistent design environment between SOLIDWORKS users.
3) User Settings
Use the User Settings page to set preferences for Toolbox operations. This is where you can determine if the Toolbox creates new configurations or new parts for each combination of component hardware options.
Files
Create Configurations: Adds a configuration to the master part file each time you use a new size of a particular component. This option creates fewer part files, but files with many configurations can grow large, which can increase assembly sizes. Also, if Toolbox is managed by SOLIDWORKS PDM, a new file version is created each time a configuration is added, potentially resulting in a large number of versions. Consider using SOLIDWORKS PDM cold storage to remove old versions from the vault.
Create Parts: Creates an individual part file each time you use a new size of a particular component. This option keeps the size of part files smaller but creates more files.
Writing to read-only documents
Always change read-only status of document before writing: Specifies that Toolbox temporarily changes the read-only attribute of a file to make a change, such as creating a configuration for a new component size. After a change is done, Toolbox resets the file attribute to read-only.
This option allows multiple users to make changes to the same document because write access occurs briefly during the change. Documents that are read-only because of user rights or security settings in your operating system are not affected.
Error when writing to a read-only document: Specifies that Toolbox cannot change read-only documents; an error message appears. Select this option when you manage Toolbox component files from a PDM system.
Part Numbers
You can assign the same part number to more than one configuration of a Toolbox part if the parts are geometrically equal. For example, you might want to change the value of a custom property but retain the same part number because the geometry is the same.
Allow duplicate part numbers for geometrically equal components: Allows you to assign the same part number to more than one Toolbox part.
Display Options
To display custom configuration names or other properties in the FeatureManager design tree or Bill of Materials, select:
Show as Component Name in FeatureManager to change the component name in the FeatureManager design tree.
Show as Part Number in Bill of Materials to change the part number in the Bill of Materials.
Show as Description in Bill of Materials to change the description in the Bill of Materials.
Then, for each customization, select from:
- Filename
- Configuration Name
- Description
- Designation
- Part Number
- Toolbox Custom Properties
4) Permissions
Use the Permissions page to create a Toolbox password and set permissions for Toolbox functions. If Toolbox is managed by PDM, ensure that you also set appropriate PDM permissions for Toolbox users.
Users can view restricted functions without the Toolbox password, but they cannot modify them.
Allow editing of Content: When cleared, the Customize Hardware page is view-only for users who are not logged in.
Allow editing of Custom Properties: When cleared, the custom properties on the Customize Hardware page are view-only for users who are not logged in.
Allow adding of parts to Toolbox: When cleared, you cannot add parts to the library of Toolbox components.
Allow editing of part numbers: When cleared, you cannot save part number settings in the Toolbox PropertyManager.
Allow editing of Configuration Name/File Name: When cleared, you cannot add or change configuration names or file names in the Toolbox PropertyManager.
User Settings
Set separately for each user: Sets options on the User Settings page separately for each user as Windows Registry values.
Allow user to change: Lets users change their own settings.
Set the same for all users: Sets options on the User Settings page globally for all users.
Smart Fasteners
Set separately for each user: Sets Smart Fastener options on the Hole Wizard and Smart Fasteners pages separately for each user as Windows Registry values.
Allow user to change: Lets users change their own settings.
Set the same for all users: Sets Smart Fastener options on the Hole Wizard and Smart Fasteners pages globally for all users.
5) Smart Fasteners
Use the Smart Fasteners page to set defaults and preferences for fasteners used with Hole Wizard holes and non-Hole Wizard holes.
Washer Sizes
Select from the options to limit the available washer types, depending on the size of the Smart Fastener.
Exact match: Limits the available types to washers that match the fastener size exactly.
Greater than tolerance: Limits the available types to hole diameters that match the fastener size within the tolerance you type.
Unrestricted: Makes all washer types available.
Automatic fastener change
You can make the fastener’s length change when the hardware stack changes and make the stack hardware size change when the fastener’s size changes.
Change fastener length to ensure minimum thread engagement: Adjusts fastener lengths to satisfy your thread engagement requirements:
- Threads beyond a nut – Adds to the fastener length to ensure that the specified number of threads protrude beyond the nut.
- x diameter into a tapped hole – Sets the minimum length a fastener engages a tapped hole, based on a multiple of its diameter.
Change stack components when fastener size is changed: Changes nut and washer sizes automatically when the fastener size changes.
Fastener to use with Non-Hole Wizard holes
You can specify the default Smart Fasteners components to use with nonstandard hole types.
Fastener to use with Non-Hole Wizard holes: Specifies the Smart Fastener for non-Hole Wizard holes when you click Browse (…) and select the fastener.
Technical Support
Get help from our team by Calling us at 800-364-1652 x 2. You can also get assistance by clicking the Technical Support button or the Email Our Experts button below.